/*--------------------------------*- C++ -*----------------------------------*\
  =========                 |
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\    /   O peration     | Website:  https://openfoam.org
    \\  /    A nd           | Version:  dev
     \\/     M anipulation  |
\*---------------------------------------------------------------------------*/
FoamFile
{
    format      ascii;
    class       dictionary;
    location    "system";
    object      functionSets;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

combustionFunctions
{
    // Not possible to test here as it needs a case with a combustion model
    //#includeFunc Qdot

    // Not possible to test here as it needs a XiFoam case
    //#includeFunc XiReactionRate
}

controlFunctions
{
    #includeFunc stopAtClockTime(stopTime=3600)

    #includeFunc stopAtFile

    #includeFunc time

    #includeFunc writeObjects(kEpsilon:G)
}

fieldsFunctions
{
    #includeFunc age

    #includeFunc components(U)

    #includeFunc CourantNo

    #includeFunc cylindrical(origin=(0 0 0), axis=(0 0 1), U)

    #includeFunc ddt(p)

    #includeFunc div(phi)

    #includeFunc enstrophy

    // !!! Takes a list of fields, not a single field like most others. It has
    // an inconsistent name convention; i.e., "<fieldName>Mean", rather than
    // "mean(<fieldName>)". It also does both "mean" and "prime2Mean". Consider
    // fixing the output field naming and splitting into separate
    // configurations for the different outputs.
    #includeFunc fieldAverage(U, k, epsilon)

    #includeFunc flowType

    #includeFunc grad(p)

    #includeFunc Lambda2

    #includeFunc MachNo

    #includeFunc mag(U)

    #includeFunc magSqr(U)

    #includeFunc PecletNo

    // Not possible to test here as it needs a multiphase case
    //#includeFunc phaseMap

    #includeFunc Q

    #includeFunc randomise(U, magPerturbation=0.1)

    #includeFunc reconstruct(phi)

    #includeFunc scale(age, scale=0.1)

    #includeFunc shearStress

    #includeFunc streamFunction

    #includeFunc surfaceInterpolate(rho, result=rhof)

    #includeFunc totalEnthalpy

    #includeFunc turbulenceFields(nuEff, R)

    #includeFunc turbulenceIntensity

    #includeFunc vorticity

    #includeFunc wallHeatFlux

    #includeFunc wallHeatTransferCoeff(rho=1.225, Cp=1005, Pr=0.7, Prt=0.9)

    #includeFunc wallShearStress

    #includeFunc writeCellCentres

    #includeFunc writeCellVolumes

    // !!! Only writes the internal parts of vol fields. The name should really
    // be less general to reflect this; e.g., writeInternalFieldsVTK. However,
    // a better change would be further library-ise the internals of foamToVTK
    // and incorporate it into this object so that it writes patches, surface
    // fields, point fields, lagrangian, etc... Then we could deprecate
    // foamToVTK in favour of this function.
    #includeFunc writeVTK(U, p)

    #includeFunc yPlus
}

fieldsOperationsFunctions
{
    // Operation sequence to compute normalised direction of velocity
    // perturbation from mean
    #includeFunc subtract(U, UMean, result=u)
    #includeFunc uniform
    (
        fieldType=volScalarField,
        field=mag(smallU),
        dimensions=[0 1 -1 0 0 0 0],
        value=1e-16
    )
    #includeFunc add(mag(U), mag(smallU), result=stabilise(mag(U)))
    #includeFunc divide(u, stabilise(mag(U)), result=uFrac)

    // Operation to compute a tensor by doing an outer vector product
    #includeFunc multiply(U, u)

    // Operation sequence to compute the log of temperature divided by an
    // ambient value
    #includeFunc uniform
    (
        fieldType=volScalarField,
        field=Ta,
        dimensions=[0 0 0 1 0 0 0],
        value=297
    )
    #includeFunc divide(T, Ta)
    #includeFunc log(divide(T,Ta))
}

forcesFunctions
{
    #includeFunc forcesIncompressible
    (
        patches=(walls),
        rhoInf=1.225,
        CofR=(0 0 0),
        pitchAxis=(0 1 0)
    )

    #includeFunc forceCoeffsIncompressible
    (
        patches=(walls),
        magUInf=20,
        lRef=1,
        Aref=1,
        CofR=(0 0 0),
        liftDir=(0 0 1),
        dragDir=(1 0 0),
        pitchAxis=(0 1 0)
    )

    #includeFunc forcesCompressible
    (
        patches=(walls),
        CofR=(0 0 0),
        pitchAxis=(0 1 0)
    )

    #includeFunc forceCoeffsCompressible
    (
        patches=(walls),
        magUInf=20,
        rhoInf=1.225,
        lRef=1,
        Aref=1,
        CofR=(0 0 0),
        liftDir=(0 0 1),
        dragDir=(1 0 0),
        pitchAxis=(0 1 0)
    )

    // Not possible to test here as it needs a multiphase Euler-Euler case
    //#includeFunc phaseForces(phase=air)
}

graphsFunctions
{
    #includeFunc graphUniform
    (
        start=(-0.5 -0.5 0),
        end=(0.5 0.5 0),
        nPoints=100,
        fields=(p U)
    )

    #includeFunc graphCell
    (
        start=(-0.500001 -0.500001 0),
        end=(0.500001 0.500001 0),
        fields=(p U)
    )

    #includeFunc graphLayerAverage
    (
        patches=(inlet),
        axis=x,
        fields=(p U)
    )
}

lagrangianFunctions
{
    // Not possible to test here as it needs a DSMC case
    //#includeFunc dsmcFields
}

numericalFunctions
{
    #includeFunc residuals(p, U, h, k, epsilon)

    #includeFunc timeStep
}

pressureFunctions
{
    #includeFunc divide(p, rho, result=kinematic(p))

    #includeFunc staticPressureIncompressible(kinematic(p), rhoInf=1.2)

    #includeFunc totalPressureIncompressible(kinematic(p), rhoInf=1.2)

    #includeFunc totalPressureCompressible
}

probesFunctions
{
    #includeFunc probes(points=((-0.2 -0.2 0) (0 0 0) (0.2 0.2 0)), p, U, T)

    #includeFunc internalProbes(points=((-0.2 -0.2 0) (0.2 0.2 0)), p, U, T)

    #includeFunc boundaryProbes
    (
        points=((-0.2 -0.2 -0.04) (0.2 0.2 -0.04)),
        maxDistance=0.02,
        p,
        U,
        T
    )

    #includeFunc uniform
    (
        fieldType=volScalarField,
        field=alpha.dummy,
        dimensions=[],
        value=0.2
    )

    #includeFunc interfaceHeight
    (
        alpha=alpha.dummy,
        points=((-0.2 -0.2 0) (0.2 0.2 0))
    )
}

solversFunctions
{
    #includeFunc scalarTransport(s, schemesField=h)

    #includeFunc phaseScalarTransport
    (
        s.dummy,
        solveAlphaPhi=yes,
        p=p_rgh,
        rho=rho,
        schemesField=h
    )

    // Not possible to test here as not compatible with compressible solvers
    //#includeFunc particles
}

streamlinesFunctions
{
    #includeFunc streamlinesSphere
    (
        centre=(0 0 0),
        radius=0.1,
        nPoints=100,
        p,
        U,
        direction=forward
    )

    #includeFunc streamlinesLine
    (
        start=(-0.5 -0.5 -0.05),
        end=(0.5 0.5 0.05),
        nPoints=100,
        p,
        U,
        direction=backward
    )

    #includeFunc streamlinesPatch
    (
        patch=inlet,
        nPoints=100,
        p,
        U
    )

    #includeFunc streamlinesPoints
    (
        points=((-0.2 -0.2 0) (0 0 0) (0.2 0.2 0))
        p,
        U,
        direction=forward
    )
}

surfaceFunctions
{
    #includeFunc cutPlaneSurface(point=(0 0 0), normal=(0 0 1), p, U)

    #includeFunc isoSurface(isoField=nut, isoValue=0.1, p, U)

    #includeFunc patchSurface(patch=walls, p, U)
}

surfaceFieldValueFunctions
{
    #includeFunc patchAverage(patch=inlet, k)

    #includeFunc patchIntegrate(patch=inlet, epsilon)

    #includeFunc patchFlowRate(patch=inlet)

    #includeFunc patchDifference(patch1=inlet, patch2=outlet, p)

    #includeFunc faceZoneAverage(faceZone=f0, U)

    #includeFunc faceZoneFlowRate(faceZone=f0)

    #includeFunc triSurfaceAverage(triSurface=mid.obj, p)

    #includeFunc triSurfaceVolumetricFlowRate(triSurface=mid.obj)

    #includeFunc triSurfaceDifference
    (
        name1=nearInlet.obj,
        name2=nearOutlet.obj,
        p
    )
}

volFieldValueFunctions
{
    #includeFunc cellMin(epsilon)

    #includeFunc cellMax(k)

    #includeFunc cellMinMag(U, writeLocation=yes)

    #includeFunc cellMaxMag(U, writeLocation=yes)

    #includeFunc volAverage(p)

    #includeFunc volIntegrate(rho)
}

$combustionFunctions;
$controlFunctions;
$fieldsFunctions;
$fieldsOperationsFunctions;
$forcesFunctions;
$graphsFunctions;
$lagrangianFunctions;
$numericalFunctions;
$pressureFunctions;
$probesFunctions;
$solversFunctions;
$streamlinesFunctions;
$surfaceFunctions;
$surfaceFieldValueFunctions;
$volFieldValueFunctions;

// ************************************************************************* //
